|
Time Period
During a static step you assign a time period to the analysis. This is necessary for
cross-references to the amplitude options, which can be used to determine the variation of
loads and other externally prescribed parameters during a step (see Amplitude Curves). In some cases
this time scale is quite real—for example, the response may be caused by temperatures
varying with time based on a previous transient heat transfer run; or the material response
may be rate dependent (rate-dependent plasticity), so that a natural time scale exists.
Other cases do not have such a natural time scale; for example, when a vessel is pressurized
up to limit load with rate-independent material response. If you do not specify a time
period, Abaqus/Standard defaults to a time period in which “time” varies from 0.0 to 1.0 over the step. The
“time” increments are then fractions of the total period of the step.
Linear Static Analysis
Linear static analysis involves the specification of load cases and
appropriate boundary conditions. If all or part of a problem has linear
response, substructuring is a powerful capability for reducing the
computational cost of large analyses (see
Using Substructures).
Nonlinear Static Analysis
Nonlinearities can arise from large-displacement effects, material
nonlinearity, and/or boundary nonlinearities such as contact and friction (see
General and Perturbation Procedures)
and must be accounted for. If geometrically nonlinear behavior is expected in a
step, the large-displacement formulation should be used. In most nonlinear
analyses the loading variations over the step follow a prescribed history such
as a temperature transient or a prescribed displacement.
Unstable Problems
Some static problems can be naturally unstable, for a variety of reasons.
Buckling or Collapse
In some geometrically nonlinear analyses, buckling or collapse may occur.
In these cases a quasi-static solution can be obtained only if the magnitude of
the load does not follow a prescribed history; it must be part of the solution.
When the loading can be considered proportional (the loading over the complete
structure can be scaled with a single parameter), a special approach—called the
“modified Riks method”—can be used, as described in
Unstable Collapse and Postbuckling Analysis.
Local Instabilities
In other unstable analyses the instabilities are local (for example, surface wrinkling,
material instability, or local buckling), in which case global load control methods such
as the Riks method are not appropriate. Abaqus/Standard offers the option to stabilize this class of problems by applying damping throughout
the model in such a way that the viscous forces introduced are sufficiently large to
prevent instantaneous buckling or collapse but small enough not to affect the behavior
significantly while the problem is stable. The available automatic stabilization schemes
are described in detail in Automatic Stabilization of Unstable Problems.
Incrementation
Abaqus/Standard uses Newton's method to solve the nonlinear equilibrium equations. Many problems
involve history-dependent response; therefore, the solution usually is obtained as a
series of increments, with iterations to obtain equilibrium within each increment.
Increments must sometimes be kept small (in the sense that rotation and strain increments
must be small) to ensure correct modeling of history-dependent effects. Most commonly the
choice of increment size is a matter of computational efficiency: if the increments are
too large, more iterations are required. Furthermore, Newton's method has a finite radius
of convergence; too large an increment can prevent any solution from being obtained
because the initial state is too far away from the equilibrium state that is being
sought—it is outside the radius of convergence. Thus, there is an algorithmic restriction
on the increment size.
Automatic Incrementation
In most cases the default automatic incrementation scheme is preferred because it selects
increment sizes based on computational efficiency.
Direct Incrementation
Direct user control of the increment size is also provided because if you
have considerable experience with a particular problem, you may be able to
select a more economical approach.
Special Cases for Direct Incrementation
With direct user control, the solution to an increment can be accepted
after the maximum number of iterations allowed has been completed (as defined
in
Commonly Used Control Parameters),
even if the equilibrium tolerances are not satisfied. This approach is not
recommended; it should be used only in special cases when you have a thorough
understanding of how to interpret results obtained in this way. Very small
increments and a minimum of two iterations are usually necessary if this option
is used.
Steady-State Frictional Sliding
In a static analysis procedure you can model steady-state frictional sliding
between two deformable bodies or between a deformable and a rigid body that are
moving with different velocities by specifying the motions of the bodies as
predefined fields. In this case it is assumed that the slip velocity follows
from the difference in the user-specified velocities and is independent of the
nodal displacements, as described in
Coulomb friction.
Since this frictional behavior is different from the frictional behavior
used without steady-state frictional sliding, discontinuities may arise in the
solutions between an analysis step in which relative velocity is determined
from predefined motions and prior steps. An example is the discontinuity that
occurs between the initial preloading of the disc pads in a disc brake system
and the subsequent braking analysis where the disc spins with a prescribed
rotation. To ensure a smooth transition in the solution, it is recommended that
all analysis steps prior to the analysis step in which predefined motion is
specified use a zero coefficient of friction. You can then modify the friction
properties in the steady-state analysis to use the desired friction coefficient
(see
Changing Friction Properties during an Abaqus/Standard Analysis).
Initial Conditions
Initial values of stresses, temperatures, field variables,
solution-dependent state variables, etc. can be specified.
Initial Conditions
describes all of the available initial conditions.
Boundary Conditions
Boundary conditions can be applied to any of the displacement or rotation
degrees of freedom (1–6); to warping degree of freedom 7 in open-section beam
elements; or, if hydrostatic fluid elements are included in the model, to fluid
pressure degree of freedom 8. If boundary conditions are applied to rotation
degrees of freedom, you must understand how finite rotations are handled by
Abaqus
(see
Boundary Conditions).
During the analysis prescribed boundary conditions can be varied using an
amplitude definition (see
Amplitude Curves).
Loads
The following loads can be prescribed in a static stress analysis:
-
Concentrated nodal forces can be applied to the displacement degrees of
freedom (1–6); see
Concentrated Loads.
-
Distributed pressure forces or body forces can be applied; see
Distributed Loads.
The distributed load types available with particular elements are described in
Abaqus Elements Guide.
Predefined Fields
The following predefined fields can be specified in a static stress
analysis, as described in
Predefined Fields:
-
Although temperature is not a degree of freedom in a static stress analysis, you can specify
nodal temperatures as a predefined field. Any difference between the applied and initial
temperatures causes thermal strain if a thermal expansion coefficient is given for the
material (Thermal Expansion). The
specified temperature also affects temperature-dependent material properties, if any.
-
The values of user-defined field variables can be specified. These
values only affect field-variable-dependent material properties, if any.
-
Although pore fluid pressure is not a degree of freedom in a static stress analysis,
you can specify nodal pore fluid pressure as a predefined field variable (see Pore Fluid Pressure). The total
stress is computed as the sum of the effective stress and the pore fluid pressure. When
the solid grains are compressible (finite bulk modulus), the effective strain is
computed as the total strain minus the volumetric strain caused by the pore pressure
acting on the solid grain.
Material Options
Most material models that describe mechanical behavior are available for use
in a static stress analysis. The following material properties are not active
during a static stress analysis: acoustic properties, thermal properties
(except for thermal expansion), mass diffusion properties, electrical
conductivity properties, and pore fluid flow properties.
Rate-dependent yield (Rate-Dependent Yield),
hysteresis (Hysteresis in Elastomers),
and two-layer viscoplasticity (Two-Layer Viscoplasticity)
are the only time-dependent material responses that are active during a static
analysis. The rate-dependent yield response is often important in rapid
processes such as metal-working problems. The hysteresis model is useful in
modeling the large-strain, rate-dependent response of elastomers that exhibit a
pronounced hysteresis under cyclic loading. The two-layer viscoplasticity model
is useful in situations where a significant time-dependent behavior as well as
plasticity is observed, which for metals typically occurs at elevated
temperatures. An appropriate time scale must be specified so that
Abaqus/Standard
can treat the rate dependence of the material responses correctly.
Static creep and swelling problems and time-domain viscoelastic models are analyzed by the
quasi-static procedure (Quasi-Static Analysis). When any of these
time-dependent material models are used in a static analysis, a rate-independent elastic
solution is obtained and the chosen time scale does not have an effect on the material
response. For creep and swelling behavior this indicates that the loading is applied
instantaneously compared with the natural time scale over which creep effects take place.
The same concept of instantaneous load application applies to time-domain
viscoelastic behavior. You can also obtain the fully relaxed long-term
viscoelastic solution directly in a static procedure without having to perform
a transient analysis; this choice is meaningful only when time-domain
viscoelastic material properties are defined. If the long-term viscoelastic
solution is requested, the internal stresses associated with each of the Prony
series terms are increased gradually from their values at the beginning of the
step to their long-term values at the end of the step.
For the two-layer viscoplastic material model, you can obtain the long-term
response of the elastic-plastic network alone.
When frequency-domain viscoelastic material properties are defined (see
Frequency Domain Viscoelasticity),
the corresponding elastic moduli must be specified as long-term elastic moduli.
This implies that the response corresponds to the long-term elastic solution,
regardless of the time period specified for the step.
Rate-Dependent Yield and Friction
You can control whether to consider or ignore the strain rate–dependence of the yield
stress and the slip rate–dependence of the friction coefficient within the step.
Elements
Any of the stress/displacement elements in Abaqus/Standard can be used in a static stress analysis (see Choosing the Appropriate Element for an Analysis Type). Although
velocities are not available in a static stress analysis, dashpots can still be used (they
can be useful in stabilizing an unstable problem). The relative velocity is calculated as
described in Dashpots.
Acoustic elements are not active in a static step. Consequently, if an acoustic-solid analysis
includes a static step, only the solid elements deform. If the deformations are large, the
acoustic and solid meshes may not conform, and subsequent acoustic-structural analysis steps
may produce misleading results. See About ALE Adaptive Meshing for information on
using the adaptive meshing technique to deform the acoustic mesh.
Output
The element output available for a static stress analysis includes stress;
strain; energies; the values of state, field, and user-defined variables; and
composite failure measures. The nodal output available includes displacements,
reaction forces, and coordinates. All of the output variable identifiers are
outlined in
Abaqus/Standard Output Variable Identifiers.
Input File Template
HEADING
…
BOUNDARY
Data lines to specify zero-valued boundary conditions
INITIAL CONDITIONS
Data lines to specify initial conditions
AMPLITUDE
Data lines to define amplitude variations
**
STEP (,NLGEOM)
Once NLGEOM is specified, it will be active in all subsequent steps
STATIC, DIRECT
Data line to define direct time incrementation
BOUNDARY
Data lines to prescribe zero-valued or nonzero boundary conditions
CLOAD and/or DLOAD
Data lines to specify loads
TEMPERATURE and/or FIELD
Data lines to specify values of predefined fields
END STEP
**
STEP
STATIC
Data line to control automatic time incrementation
BOUNDARY, OP=MOD
Data lines to modify or add zero-valued or nonzero boundary conditions
CLOAD, OP=NEW
Data lines to specify new concentrated loads; all previous concentrated
loads will be removed
DLOAD, OP=MOD
Data lines to specify additional or modified distributed loads
TEMPERATURE and/or FIELD
Data lines to specify additional or modified values of predefined fields
END STEP |